Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 561)

Grooving/Cutoff Cycles
Chapter 23
23-7
The format for this cycle is:
G77X__Z__I__K__F__D__;
Where : Is :
Z__ the location where the last groove is cut. If only one groove is to be cut do not
program Z. This may be programmed as either an incremental or absolute value.
X__ the total depth of the groove from the X coordinate position of the tool prior to the
execution of the G77 block. If this cycle is to be used as a cut off cycle the depth
programmed here should drive the tool through the center or inside diameter of the
part. If a cut off is being made from the inside of the part, it should drive the tool
beyond the outside diameter of the part. This value represents the location of the
bottom of the groove cut. It may be programmed as either an incremental or
absolute value and is also affected by radius or diameter mode (G07 or G08).
K__ the distance between each groove. If the distance between the location of the last
groove (programmed with Z) and the next to the last groove is less than the value
programmed with K, then the K value is not used to determine the position of the
last groove. The last groove is always cut at the location programmed with Z. The
K parameter is always programmed as an incremental value regardless of the
current mode of the control.
I__ the amount that the cutting tool infeeds into the workpiece with each step. The step
is followed by a retract of amount e (set in AMP by the system installer). The
cutting tool then infeeds into the workpiece an amount I + e, retracts an amount e,
infeeds I + e, retracts e, etc. This repeats until the total programmed depth of the
groove X is reached. When this depth is reached the cutting tool stops infeeding
and either shifts an amount D (if programmed) or retracts to the starting coordinate
at rapid feedrate. The I-word is always programmed as an incremental value
regardless of the current mode of the control.
F optional in the grooving block. If programmed the value entered with this parameter
replaces the currently active feedrate used when infeeding into the part. If F is not
programmed the currently active feedrate is used.
D__ the size of the incremental shift move made by the tool when the full depth of a cut
off has been reached. This parameter must be programmed even if its value is zero
when not using this cycle as a cutoff. A value other than zero is assigned to D only if
the grooving cycle is being used as a cut off cycle. It is always an incremental value
regardless of the current mode. The sign of the value programmed with the D
parameter determines the shift direction and should move the tool away from the
part. Programming this shift during a cutoff move helps to provide a good finish
since the cutting tool is not touching the part when it is retracted at the rapid
feedrate.
CAUTION: The shift programmed with a D parameter is
executed as a rapid move. Make sure that the cutting tool is
clear to shift at the end of the grooving cycle.